In structural mechanics, the equations relating stress and strain
arise from the balance of forces in the material medium. *Plane stress* is
a condition that prevails in a flat plate in the *x*-*y* plane,
loaded only in its own plane and without *z*-direction
restraint.

The stress-strain relation can then be written, assuming isotropic and isothermal conditions

$$\left(\begin{array}{c}{\sigma}_{x}\\ {\sigma}_{y}\\ {\tau}_{xy}\end{array}\right)=\frac{E}{1-{\nu}^{2}}\left(\begin{array}{ccc}1& \nu & 0\\ \nu & 1& 0\\ 0& 0& \frac{1-\nu}{2}\end{array}\right)\left(\begin{array}{c}{\epsilon}_{x}\\ {\epsilon}_{y}\\ {\gamma}_{xy}\end{array}\right),$$

where *σ _{x}* and

The deformation of the material is described by the displacements
in the *x* and *y* directions, *u* and *v*,
from which the strains are defined as

$$\begin{array}{c}{\epsilon}_{x}=\frac{\partial u}{\partial x}\\ {\epsilon}_{y}=\frac{\partial v}{\partial y}\\ {\gamma}_{xy}=\frac{\partial u}{\partial y}+\frac{\partial v}{\partial x}.\end{array}$$

The balance of force equations are

$$\begin{array}{c}-\frac{\partial {\sigma}_{x}}{\partial x}-\frac{\partial {\tau}_{xy}}{\partial y}={K}_{x}\\ -\frac{\partial {\tau}_{xy}}{\partial x}-\frac{\partial {\sigma}_{y}}{\partial y}={K}_{y},\end{array}$$

where *K _{x}* and

Combining the preceding relations, we arrive at the displacement equations, which can be written

$$-\nabla \xb7\left(c\otimes \nabla u\right)=k,$$

where **c** is a rank four tensor
(see c Coefficient for Systems), which can be
written as four 2-by-2 matrices *c*_{11}, *c*_{12}, *c*_{21},
and *c*_{22}:

$$\begin{array}{c}{c}_{11}=\left(\begin{array}{cc}2G+\mu & 0\\ 0& G\end{array}\right)\\ {c}_{12}=\left(\begin{array}{cc}0& \mu \\ G& 0\end{array}\right)\\ {c}_{21}=\left(\begin{array}{cc}0& G\\ \mu & 0\end{array}\right)\\ {c}_{22}=\left(\begin{array}{cc}G& 0\\ 0& 2G+\mu \end{array}\right),\end{array}$$

where *G*, the *shear modulus,* is
defined by

$$G=\frac{E}{2\left(1+\nu \right)},$$

and *µ* in turn is defined by

$$\begin{array}{l}\mu =2G\frac{\nu}{1-\nu}.\\ k=\left(\begin{array}{l}{K}_{x}\\ {K}_{y}\end{array}\right)\end{array}$$

are *volume forces.*

This is an elliptic PDE of system type (*u* is
two-dimensional), but you need only to set the application mode to **Structural
Mechanics, Plane Stress** and then enter the material-dependent
parameters *E* and *ν* and
the volume forces **k** into the PDE
Specification dialog box.

In this mode, you can also solve the eigenvalue problem, which is described by

$$\begin{array}{c}-\nabla \cdot (c\otimes \nabla u)=\lambda du\\ d=\left(\begin{array}{cc}\rho & 0\\ 0& \rho \end{array}\right).\end{array}$$

*ρ*, the density, can also be entered
using the PDE Specification dialog box.

In the Plot Selection dialog box, the *x*-
and *y*-displacements, *u* and *v*,
and the absolute value of the displacement vector (*u*, *v*)
can be visualized using color, contour lines, or *z*-height,
and the displacement vector field (*u*, *v*)
can be plotted using arrows or a deformed mesh. In addition, for visualization
using color, contour lines, or height, you can choose from 15 scalar
tensor expressions:

$${u}_{x}=\frac{\partial u}{\partial x}$$

$${u}_{y}=\frac{\partial u}{\partial y}$$

$${v}_{x}=\frac{\partial v}{\partial x}$$

$${v}_{y}=\frac{\partial v}{\partial y}$$

`exx`

, the*x*-direction strain (*ε*)_{x}`eyy`

, the*y*-direction strain (*ε*)_{y}`exy`

, the shear strain (*γ*)_{xy}`sxx`

, the*x*-direction stress (*σ*)_{x}`syy`

, the*y*-direction stress (*σ*)_{y}`sxy`

, the shear stress (*τ*)_{xy}`e1`

, the first principal strain (*ε*_{1})`e2`

, the second principal strain (*ε*_{2})`s1`

, the first principal stress (*σ*_{1})`s2`

, the second principal stress (*σ*_{2})`von Mises`

, the von Mises effective stress$$\sqrt{{\sigma}_{1}^{2}+{\sigma}_{2}^{2}-{\sigma}_{1}{\sigma}_{2}}.$$

For a more detailed discussion on the theory of stress-strain
relations and applications of FEM to problems in structural mechanics,
see Cook, Robert D., David S. Malkus, and Michael E. Plesha, *Concepts
and Applications of Finite Element Analysis*, 3rd edition,
John Wiley & Sons, New York, 1989.

Consider a steel plate that is clamped along a right-angle inset at the lower-left corner, and pulled along a rounded cut at the upper-right corner. All other sides are free.

The steel plate has the following properties: Dimension: 1-by-1
meters; thickness 1 mm; inset is 1/3-by-1/3 meters. The rounded cut
runs from (2/3, 1) to (1, 2/3). Young's modulus: 196 · 10^{3} (MN/m^{2}),
Poisson's ratio: 0.31.

The curved boundary is subjected to an outward normal load of
500 N/m. We need to specify a surface traction; we therefore divide
by the thickness 1 mm, thus the surface tractions should be set to
0.5 MN/m^{2}. We will use the force unit MN
in this example.

We want to compute a number of interesting quantities, such
as the *x-* and *y-*direction strains
and stresses, the shear stress, and the von Mises effective stress.

Using the PDE app, set the application mode to **Structural
Mechanics, Plane Stress**.

The CSG model can be made very quickly by drawing a polygon
with corners in `x = [0 2/3 1 1 1/3 1/3 0]`

and ```
y
= [1 1 2/3 0 0 1/3 1/3]
```

and a circle with center in ```
x
= 2/3, y = 2/3
```

and radius `1/3`

.

The polygon is normally labeled P1 and the circle C1, and the CSG model of the steel plate is simply P1+C1.

Next, select **Boundary Mode** to specify the
boundary conditions. First, remove all subdomain borders by selecting **Remove
All Subdomain Borders** from the **Boundary** menu.
The two boundaries at the inset in the lower left are clamped, i.e.,
Dirichlet conditions with zero displacements. The rounded cut is subject
to a Neumann condition with `q = 0`

and ```
g1
= 0.5*nx
```

, `g2 = 0.5*ny`

. The remaining
boundaries are free (no normal stress), that is, a Neumann condition
with `q = 0`

and `g = 0`

.

The next step is to open the PDE Specification dialog box and enter the PDE parameters.

The *E* and *ν* (`nu`

)
parameters are Young's modulus and Poisson's ratio, respectively.
There are no volume forces, so `Kx`

and `Ky`

are
zero. ρ (`rho`

) is not used in this mode. The
material is homogeneous, so the same *E* and [[ν
apply to the whole 2-D domain.

Initialize the mesh by clicking the Δ button. If you want,
you can refine the mesh by clicking the **Refine** button.

The problem can now be solved by clicking the **=** button.

A number of different strain and stress properties can be visualized,
such as the displacements *u* and *v*,
the *x-* and *y-*direction strains
and stresses, the shear stress, the von Mises effective stress, and
the principal stresses and strains. All these properties can be selected
from pop-up menus in the Plot Selection dialog box. A combination
of scalar and vector properties can be plotted simultaneously by selecting
different properties to be represented by color, height, vector field
arrows, and displacements in a 3-D plot.

Select to plot the von Mises effective stress using color and
the displacement vector field (*u*,*v*)
using a deformed mesh. Select the **Color** and **Deformed
mesh** plot types. To plot the von Mises effective stress,
select `von Mises`

from the pop-up menu in the **Color** row.

In areas where the gradient of the solution (the stress) is
large, you need to refine the mesh to increase the accuracy of the
solution. Select **Parameters** from the **Solve** menu
and select the **Adaptive mode** check box. You can
use the default options for adaptation, which are the **Worst
triangles** triangle selection method with the **Worst
triangle fraction** set to 0.5. Now solve the plane stress
problem again. Select the** Show Mesh** option
in the Plot Selection dialog box to see how the mesh is refined in
areas where the stress is large.

**Visualization of the von Mises Effective Stress
and the Displacements Using Deformed Mesh**

Was this topic helpful?